datum feature interpretation

datum feature interpretation

datum feature interpretation

I sent a RFQ for a wrench to a Chinese vendor. This vendor has made similar wrenches for us before. We are basically brand new to using GD&T. I know that this vendor has seen GD&T before but I do not know their level of expertise (especially w.r.t. ASME Y14.5-2009).

The vendor's proposed changes are on the attached drawing. Their feedback is in yellow. What I would like to discuss is their replacement of my profile tolerances on the square boss and square hole with position tolerances (as seen in the upper most view). Of course, what I am after is that both square features are oriented to each other to maintain a nominally uniform wall thickness between the boss and the hole and that both square features are centered on the part.

While I believe that the proposed position tolerances still achieve this I am wondering if the interpretation of what datum feature "E" is has changed. With the original profile tolerance datum feature "E" is the square hole. Does using the 2X Ø.510 as datum feature "E" achieve the same thing? Does anyone read that datum feature "E" is only one set of opposed surfaces and not both sets of opposed surfaces?

I am thinking that I will add a note to the datum feature symbol stating that datum feature "E" is the square hole just to be safe.

RE: datum feature interpretation

They don't like profile......
As shown now. E is only the horizontal middle plane.
I would make the flat surface (top of the square boss/hole) datum feature A (give it some flatness) and put a perpencicularity within some tolerance to A for the vertical dimension .510 and call it datum feature E. Then
another perpendicualrity for the horizontal .510 to A primary and E secondary and call it D. Then the side bosses will be positioned to A, E and D
Make .510 and .860 direct toleranced dimensions not basic.
Corner radii are not controlled for both square boss and square hole. I guess you have to make them ± and put some tolerance (if the title block is not acceptable)

If they don't like the profile ...they don't like the profile.....nothing you can do......
yes, you can educate them.....

Not sure what was before ±.020 supplier proposal for the size tolerance (not part of what you want to discuss)

RE: datum feature interpretation

Yes, my initial thought was that they just don't like/understand profile. However, they did not ask for a change to the profile tolerances on the side relief cut (from points y to z) or the dimple indentations inside the square hole. Maybe that's just b/c they knew they couldn't replace these with position.

What I did not state earlier is that I also created supplemental "explanation" drawings that describe the tolerance zones required by the FCFs on the part drawing. I made these b/c there are many internally that do not fully understand GD&T yet and also b/c we were worried that the vendor might not understand also. So any question they might have had on the profile tolerances should have been answered (if I did a good job on the explanation docs). I'm wondering if they can simply measure position easier than profile.

Yes, I realize that some originally basic dims will require tolerance when we switch from profile to position.

greenimi - If I add the note "square hole" to datum feature symbol for datum E do you think that clears up what the datum feature actually is?

RE: datum feature interpretation

1. Regardless of how the datum feature E is going to be interpreted according to the vendor's proposal, I hope you realize that this will leave the boss and the hole uncontrolled in terms of their size and form.

2. There is a slot at the bottom of the part (its width has been assigned datum feature C). From functional standpoint, is it acceptable that the square boss and hole can be at any angular orientation relative to C?

RE: datum feature interpretation

In my opinion: square symbol and square definition is valid for a dimension and not for datum features. 3.3.16--The symbolic means of indicating that a single dimension applies to a square shape shall be to precede that dimension with the square symbol,
I do not know if you can extend it to the datum feature.

RE: datum feature interpretation

Do you want to establish your primary datum feature as a complex feature? Or like a linear extruded shape? similar with option g or f respectivelly (page 50)? If yes, both of them have profiles to define the datum feature.
Probably you want two mutual perpendicular planes, but no corner radii to be included.

RE: datum feature interpretation

Thanks for all the responses. I'll go in order.
------------------
pmarc -
1) I believe that rule #1 will control size and form for the square boss and square hole. Once I remove the basic dimension from them they will be +/-.015 per the title block.
2) Yes the square boss and square hole can have any orientation w.r.t. the opening (datum feature C) as long as they maintain their orientation to each other. The design intent of the part allows for this. A ratchet interfaces with the square hole. There is no needed orientation between the ratchet and the wrench.
-----------------------
greenimi –
1) I would tend to agree with you about the use of the square symbol. OK for dimensions but not for datum feature identification.
2) I am looking for two perpendicular planes to be created by using the square hole as a datum feature. Are you saying that the inclusion of the 4 corner radii in my original profile tolerance will yield something else? If so, going to the proposed position tolerances should fix this. The main goal of calling the square hole a datum feature was to be able to constrain the spherical indentations inside the square hole to be centered in-between their adjacent walls, as well as, control their size and shape. The design intent allows them to float up and down independently of each other. The ratchet will only interface with one spherical indentation. Therefore, they do not need to align with each other vertically.

RE: datum feature interpretation

As far as I can tell, neither the original nor the proposed tolerances even come close to ensuring a proper interface for a standard square drive socket wrench. Perhaps that's not the goal though, and it wasn't the question, so moving on...

The proposed datum feature E would be both pairs of opposed surfaces. ASME Y14.5-2009 paragraph 4.12.4 provides the somewhat ambiguous interpretation. In any case, it will be different from the the original version with profile all around because the radii will no longer be involved.

If you want to further clarify that four surfaces are involved, you could dimension and tolerance each opposed pair separately. Assign a separate datum feature reference letter to each, and then reference both separated by a dash as paragraph 4.12 describes.

If you replace the four spherical indentations with a single interrupted torus surface, then perhaps you could use the maximum inscribed cylinder of the square hole as the datum feature.

RE: datum feature interpretation

My initial thought is that I would replace the profile tolerance on the square hole with 2 position tolerances. One on each set of opposed surfaces. Each set of opposed surfaces would be a datum feature (E & F). The spherical indentations would have profile tolerances w.r.t. E-F only.

In a perfect world, where my vendor did not have issues with profile, I think I would look at using composite profile on the square boss and hole to address the fit of the socket drive and keeping the features centered on the part.

RE: datum feature interpretation

If the square hole is dimensioned for size (say .510 ± .015) with a square symbol for size dimension and then a phantom circle is drawn as a maximum inscribed circular element/ inscribed phantom circle and position feature control frame was associated with it (actual mating envelope), wouldn’t this accomplish the design intent without using the “ill-fame” profile?
I am trying to use irregular datum feature of size linear extruded approach.

Then the square boss will be located relative to the square hole based on the initial design intent (Quote:"Of course, what I am after is that both square features are oriented to each other to maintain a nominally uniform wall thickness between the boss and the hole and that both square features are centered on the part.")

RE: datum feature interpretation

pmarc - Attached is the current drawing. The problem that you address is still present.

possible fixes:
1) Change position FCFs of square hole to zero at MMC.
2) Compound profile control for square hole.

The vendor has already informed that they do not like profile on this feature (I don't know exactly why). Its too bad b/c this (compound profile) yields exactly what I want, tight size and shape control with more freedom for location/orientation error.

RE: datum feature interpretation

I don't think the problem is still present (or I should say, it is present but only within certain limits). Both .510 widths are controlled with position tolerances that use the same datum, at the same material boundary, thus are subject to simultaneous requirement and thus the angle between both widths is limited to a certain extent.

One more thing:
Because the square features are no longer dimensioned with basic dimensions, the 4X basic dimension locating the spherical indentations on section A-A should rather be from the center line of the square hole not from its side.

RE: datum feature interpretation

If the square hole is made at its smallest size tolerance (.500 x .500) and both sets of opposed parallel surfaces use all of their position tolerance in orientation error (in opposing angles) you are left with a effectively smaller square hole than .500 x .500 - that is my concern.

I am thinking that no matter what type of control I end up putting on this drawing that I will have the QA staff put a requirement in their inspection documentation that a standard 1/2" square socket drive should interface with our part or it is not to print. Now whether you understand GD&T or not there is no issue understanding what is required of the part. (cheapest gage ever!)

RE: datum feature interpretation

Quote (pmarc)

on your latest sketch, what prevents the square features from being produced as rhombuses (parallelograms with sides of approximately equal length but with no right angles)?

pmarc,
This was the latest sketch back then:

I have a follow up question, if you don't mind: why the parallelogram's sides perpendicularity is not restricted by the 90 degrees implied angle and the title block tolerance angle? As I can see the title block has a default angle tolerance and the default 90 angle is known.

RE: datum feature interpretation

Quote (pmarc)

The open point would then be what "standard 1/2" square socket drive" really means.

ASA B5.38? ISO 1174? IS 7214? IS 7996? DIN 3120? DIN 3121? There sure are a lot of options...

Quote (AndrewTT)

pmarc - Attached is the current drawing. The problem that you address is still present.

possible fixes:
1) Change position FCFs of square hole to zero at MMC.
2) Compound profile control for square hole.

Position tolerances of zero at MMC sound like a reasonable approach to me, especially since profile apparently won't fly. You'd probably want to do this without datum feature references to avoid creating an overly-restrictive requirement. The scheme used for datum feature A in ASME Y14.5-2009 Fig. 4-24 should work, along with other tolerances to control the relationship to the rest of the part. These could be combined into a composite FCF if desired.

Side note: Datum feature D seems awfully short for use as a primary datum feature, especially if it might have significant form error.

pylfrm

RE: datum feature interpretation

plyfrm - I was thinking position of .000 @ MMC to datum D at MMB for each set of opposed parallel surfaces of the square hole (to avoid being overly restrictive).

Originally I was going to use the entire large cylinder as a datum feature. Then we scanned similar wrenches that we had from that supplier. They are more banana shaped then a true cylinder. That is why I broke up the cylinder into smaller chunks. Really I only need the opening that interfaces with the part-to-be-installed to be centered to the lower end of the cylinder and the socket-interface to be centered to the top of the cylinder.

RE: datum feature interpretation

I didn't specify, but I was actually thinking that datum feature D seems awfully short for use as primary when referenced RFS. For instance if the length is .200 and the diameter is toleranced as 1.800 +/- .010, then the actual part surface could be spherical. This would make it incapable of constraining orientation, and the remaining translational constraint would not be very meaningful.

If referenced at MMB, form error isn't even required for the same problem to show up. The actual size just needs to be sufficiently smaller than the MMB size. An actual diameter of 1.798 would be small enough with my example dimensions.

EDIT: 1.798 was 1.978

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.The Eng-Tips staff will check this out and take appropriate action.

Additive manufacturing, also known as 3D printing, is quickly becoming an industry standard for product manufacturing in a variety of applications, including medical devices, aviation and aeronautics parts, and transportation components. Download Now